Autorouting has come a long way in the last few years. You can now buy routing software that can correctly route the most complicated boards. They aren't always fast (especially on an old '386 PC) and the best stand alone routers are usually rather expensive. Another drawback is one of modifications to a circuit. Since an autorouted board usually uses more space than a manually routed board, changes can be very difficult, as can adding those last few traces that the autorouter didn't get in.

Even if you plan on autorouting your design it is good practice to lay out your power and ground structure before starting. You should attempt to keep a "rail" structure when possible, with parallel ground and power traces between the rows of IC's. You should use a wide trace width for these runs: .050" for power and .100" for ground. Use of .025" traces to connect each part to the rail is usually sufficient, but remember to do the calculations to make sure it is enough. Good routing strategy usually calls for traces on one side of the board to be vertical with the other side horizontal, so be sure to observe this when routing your power structure. You should also flag these traces as fixed so the autorouter doesn't rip them out and route them as it wants to.

You will need to decide on the parameters for the signal traces. Even though a good board shop can manufacture with .004" lines on .008" centers (for .004" space between traces), it is probably overkill (and a lot of extra expense) for the double sided board we are talking about here. A traditional value for a double sided board is to use a .013" trace on a .025" grid (.012" space). This allows plenty of tolerance for the manufacturing shop to work with and will be cheaper and quicker than a more stringent trace width. Your autorouter will have some method for assigning these values. Some can even assign different values for different signals, useful for analog or power designs.

When routing a signal it is always a good idea to make the trace as short and direct as possible. Although it may be possible to route a board with all signal traces starting and ending on a component pad, it would probably give you a trace that snakes around so much that the function of the circuit is degraded. The solution to this is to use a pad without any component lead thru it, called a via or feed-thru. ECAD software will allow you to start a route at a pad, "stitch" to the other side of the board using a via, switch directions and complete the route at the other end of the signal. This allows better routing of the board by maintaining the vertical/horizontal strategy. Although it is a matter of pride to professional designers to minimize the via count, via use leads to better designs.

The autorouter will require information on the via pad you want to use. For a design such as we are discussing, you can use the smallest component pad on the design as a via. Since a common pad size is .062" (with a .038" hole size), this is often used for the via size. Smaller values can be used, but since board manufacturers factor the number of different hole sizes when they quote you a price it may be a good idea to keep the number of different sizes to a minimum.

It is a good idea to route critical signals by hand. This allows the signal to be routed with less bends and vias than if the autorouter does it. Some signals may require special treatment such as grounding or specific lengths that may be easier to do before autorouting than after. These traces should be flagged as fixed so the autorouter doesn't move them.

After the parameters you want to operate under are set, start the router. Since the exact procedure used by a particular program will vary it is up to you to experiment and work out any problems. It will take a while to learn all the options to a good router, have patience, RTFM, and experiment. Allow plenty of time for the router to work. It is not uncommon for a moderate design to take 12 hours to route.

When the autorouter is done you will need to find out what signals didn't route and complete them. Most ECAD programs have some sort of "slide" command to push traces out of the way, if yours doesn't you will have manually re-route traces you want moved out of the way. Keep an eye out for areas you can reroute to make more space as you are routing those last traces. Be patient and you will be done. An autorouter will usually route using more vias and trace jogs than a human, so you can usually clean up enough of the "extra stuff" to fit your line in. Remember Paretto's law: 10% of any job requires 90% of the effort. If your board was routed to 90% by the router it will take awile to shove that last 10% in.

After you are done with the routing you will want to clean up some of the glitches that any autorouter throws in. Some packages have a "gloss" mode that will automatically get rid of excessive jogs or other router "artifacts." Others will require you to look over the design and straighten things out manually.

You should now prepare a dimensioned fabrication drawing. The fabrication drawing should show the dimensions of the board in reference to the datum tool hole. It should also show a graphic representation for each hole on the board, using a different symbol for each hole size and including a table showing the quantity of each hole size. This drawing will be used by the board manufacturer in addition to the data files generated in the post-processing phase.

You may also need to create an assembly drawing to aid in building and repairing the board. This should show the outlines of the parts on the board, including their reference designators. It also should contain any special assembly instructions, such as mounting hardware and connector shells. Many companies require these drawings, others just use copies of the silkscreen legend.

The first step is printing the fabrication and assembly drawings. This may be as easy as printing them on a laser or dot-matrix printer to generating pen or photoplot files the manufacturer can use. The choice is up to you, based on the manufacturer's capabilities and your customer's requirements. It is always a good idea to look at all your data files, using a viewer program or printing them out before they are sent out.

The second step is generating the NC drill file of hole positions. This file is in ascii (usually) so that the drilling machine or human can read it to produce your board. The manufacturer will use this data to set up for drilling your boards, or may optically input the data if you can not give them a drill file. Note that it is more expensive and error prone to use the manual method. Generate a drill file whenever possible.

The third step is generating the artwork for the board. Each "layer" of the finished board must have a master artwork with opaque features on a clear background. The manufacturer will use copies of these master artworks to build the board.
This step may be done by pen plotting on matte mylar at a magnified scale, then sending the plots to a reprographic company who will photographically reduce the plot on clear film. Some people have also had some luck printing the artwork files actual size, using a laser printer and clear acetate film. The most accurate method is to generate photoplot files (also known as "gerber" files, after the manufacturer of the first photoplotters) for each layer required by the manufacturer.
You should always look at the artworks very carefully before releasing them to the manufacturer or your customer. This is the final chance you will have to check everything out before the boards are made, it is MUCH less expensive to catch a mistake here than after the boards are made.

You may have to set up an aperture file to generate photoplot files. This file tells the plotter which machine code is used for a particular size dot on the film. Although the ECAD program should produce this automatically you might want to familiarize yourself with the process so you'll know what they are asking if the manufacturer calls you with a question.

It is becoming more common for board manufacturers to have photoplotters available, you may be able to print the artworks for inspection, (or inspect them with a viewer and error checking program), then send the files directly to the manufacturer for processing by modem or FTP. This is more accurate since you don't have to worry about the film expanding or shrinking with temperature and humidty variations. You usually can save some time this way, since the manufacturer can use a Computer-Aided Manufacturing (CAM) program to set up your design using these files.